question in solidworks drawings

if i created a 2d drawing from a 3d file in solidworks, and later on changed either the directory or the name of the 3d file, when i open the file of 2d drawing i find that all the views disappears and some hash lines are created instead, is there any way of fixing this without having to redraw the 2d file of this part all over again?

i just mean for example if i created a 3d file with name xyz.sldprt and then in this file i click file, make drawing and then created the 2d file in solidworks drawing. After that i changed the name od the xyz.sldprt to abc.sldprt and open again the drawing file i already created previously i will find that the file is missing all the drawings how can i update it again to read the 3d file that i changed it's name.

I found a solution to this so i am sharing with anyone who needs help, first open solidworks, press tools then solidworks explorer and then open any part or drawing or any file in solidworks and then you can rename or change location and update all other files using this file as a refrence

Whilst using Solidworks Explorer to rename your files is the best way of doing that, when opening the drawing file and the system prompts you to the fact that it can not find the required Solid Model file, simply navigate your way to the renamed solid file and select it. SW should figure out pretty darn quick that the internal ID's found will match the drawing and rebuild the drawing again.
As for your Post #2, not everyone hangs around forums waiting to answer questions! Should have some more patience!

Broby gave a solid answer on how to do this through Solidworks Explorer. There is another way, and I still use this from time to time.
When you produce a 2D drawing in SW, it looks for the exact 3D file name of the part. If you subsequently change the name of the part or move it, the 2D drawing can't find associate the data to fill in the 2D drawing details. A brute force way to do this is to change the name of the 3D part back to the old name and put it back in the old location. You can change the name and location of the 3D file, but.....see below.

A way to avoid these problems, is to NEVER do any work on a 2D drawing unless the 3D part or assy is OPEN at the same time. While working in this mode, you are insuring that whatever you do by renaming or relocating the 3D file, the 2D drawing is sitting there re-associating these changes. After saving the 3D and 2D docs, everybody is happy and moving forward.

Right click on the drawing file name and select the References tab from a SolidWorks Open window.. From there you will be able to redirect the program to look where the part and assembly files are located. Never move or rename an active part, assembly or drawing from Windows explorer. Always use SolidWorks Explorer. You can move files and the related components using Pack&Go, to a zip file or just use SolidWorks Explorer.

By the way, you cannot just send a SolidWorks drawing to someone, you do have to include the parts. Again, Pack&Go is the best option.

When you produce a 2D drawing in SW, it looks for the exact 3D file name of the part. If you subsequently change the name of the part or move it, the 2D drawing can't find associate the data to fill in the 2D drawing details. A brute force way to do this is to change the name of the 3D part back to the old name and put it back in the old location. You can change the name and location of the 3D file, but.....see below.

A way to avoid these problems, is to NEVER do any work on a 2D drawing unless the 3D part or assy is OPEN at the same time. While working in this mode, you are insuring that whatever you do by renaming or relocating the 3D file, the 2D drawing is sitting there re-associating these changes. After saving the 3D and 2D docs, everybody is happy and moving forward.

Hope this helps.

Click to expand...

Actually, that first statement is not entirely true. SW will look for the filename that is "referenced" by the drawing, that could be any filename, not one that is the same as the drawing name... otherwise how do you explain how drawings of assemblies work?

As for the second statement, the referenced model/assembly is always opened (could be lightweight) as a hidden item when opening a drawing. I found this out when writing some VBA and realised all that I needed to do when dealing with the model referenced in the drawing, was to set the visible status to True.

The latest version of SW does allow you save a "Detached drawing" (i.e. stand alone) version of a drawing that can then be sent off to someone else.

Basically, using SW Explorer is the way to go for renaming your files, all internal links are then maintained and fixed for you without hassle, especially useful if you remember to tick the "Find all Drawings" checkbox.

SW install process should actually install a right click Solidworks Menu that allows fast access to "Pack and Go", "Rename", "Replace" and "Move" commands.
A fast way of using the same functionality as in SW Explorer.

You have to rename the original .sldprt file to it's original name and replace it in it's original directory.
There are many things you have to watch for in Assemblies and drawings like this.
If you open the raw .slddrw, it should ask you if you want to find the referenced sldprt file; say yes and point
(browse) to where the original file is even if the name if different.
-Christian

Be aware that I have advised a serious bug which can occur when copying and renaming files as described.
If you have a sheet metal part which has a reference it thinks is out of context, it can create a part which looks and measures ok, the folded drawing dimensions are correct but the developed flat pattern is wrong.
The little ? in the browser is the only warning of out of context, even if SW has lost the reference itself!
So far this bug has cost me a couple of grand by cutting profiles which were incorrect.
If you can't trust your CAD system what damn use is it?
I am sick of SW losing references, mates and dimensions ( and constantly crashing)

Hello,
In SolidWorks drawings file keep internal references to 3D models files that are used for viewing. If you change the name of the 3D files you must update these references. You can update references in SolidWorks open window where you have a button references. Select drawing file and press this button before you open the drawing file and change the reference.
To rename a 3D file don't use explorer classic rename function. Right click (in explorer) 3D file and you have there an option "SolidWorks->Rename". That function open a dialog box where you must mark "Update where used".